X5 Transform Operation Problem

[Tinhman]

Guys, i am having problem with X5 Transform/rotate operation with X5 and i wonder What am i missing here.??? Please help.

I am trying to transform/rotate only one contour and expecting to see G54 and G55 come out in my program but it is NOT.

This is My Operation Parameters

Types and Methods:

Type: Rotate

Method: Coordinate

Source: NCI

Group NCI output order: Opearation type

Copy source operation: Box Checked

Disable posting.......: Box checked

Work offset numbering:

Assign new: box checked

start: 0

increment: 1

 

But i did not have G55 in my program?? What did i do wrong??, it was OK in X4

Thanks in advance

[gcode]

what post are you using?

if its mpmaster, check Misc setting #9

[Paul Decelles]

Method: Coordinate

 

Switch this to Tool plane if you want the work offset to increment. I'd suggest reading the help for a clearer explanation of the various settings available.

[Tinhman]

Thanks for the reply.

 

To gcode:

Post base on mpmaster with some modified by IHS.

Misc #9 (Lock on First WCS [0=No,1=Yes]) set to 0

 

To Paul:

This is vertical machine and we are not using 4th axis in this case so we do not want any A (Rotation) in this program.

 

Could you please try this and let me know if you get G55 come out in your program.

Draw a rectangle then pick any end mill and cut the OD profile, then use transform operation to rotate this tool path 180 degree for second part. And you should have G54 for the first part, G55 for the second part.

 

 

 

I just tried with X4mu3 and it is OK but i could get it done with X5.

Thanks for your time.

[Chris Rizzo]

Switch this to Tool plane if you want the work offset to increment

 

what he said. you will not get an A move if you rotate about source view. Rotate by coordinate is usually used for geometry based rotations, like teeth on a gear or bolt circle type affair.

[Tinhman]

Chris,

Yes, you are right. If i rotate about source, i will not get any A move in my program. But still, I did not get my G55 to post out.

Could somebody please, please try it with X4mu3 and X5 and give me the answer??

I just want to know what did i do wrong???

Thanks in advance

[Stan_z]

hey

use -1 for start

and 2 for increment

 

not sayin its right but it posts out correctly (g54 and g55 displayed)using the mpmaster in X5

[Tinhman]

I know.

Can i call it a Bug Sir??

 

Start with 0 ( Should get G54 for the first instant)

Increment 1 ( the next instant should be G55)

 

Stan_z did you try it with X4??

 

Thanks for your time.

[Stan_z]

X4 worked Fine....so i would say a BUG

 

 

I know.

Can i call it a Bug Sir??

 

Start with 0 ( Should get G54 for the first instant)

Increment 1 ( the next instant should be G55)

 

Stan_z did you try it with X4??

 

Thanks for your time.

[neurosis]

Choose the transformation Method.

 

Tool plane transforms the selected operations in a different orientation than the original and transforms the tool axis with the operation. An operation's tool plane contains both an origin and a view. You can choose to change the origin along with the view or keep the origin stationary when Mastercam transforms/copies the tool plane. If you keep the origin stationary, Mastercam transforms only the tool plane's view. The Tool plane option also activates Work offset numbering parameters so that you can output a different work offset with each new tool plane.

 

Coordinate computes new coordinates for the transformed operation in the same tool plane as the original operation.

 

 

The way this reads from the help file, "Tool Plane" activates the work number offset parameters for your different fixture offsets.

 

If it works in X4 maybe the bug was in X4? Have you tried as mentioned twice already above and try the tool plane method? Ive always used "Tool Plane" when separate fixture offsets are required.

 

:shrug:

[Tinhman]

tried it again with tool plane method, still no go.

 

 

Thanks for the reply Neurosis.

Please do me a favor sir. Try it and let me know if everything it woking OK on your end.

Thanks in advance

[Dan@home]

Worked for me when I used 90 deg and 270. Although I did get C-axis moves ,as it should.

[Tinhman]

Thanks for your time Dan.

But the machine should be 3 axis vertical and the rotation should be about top view from 0 to 180 deg. for the second part. please try it again and let me know.

Thanks

[neurosis]

I understand what you are trying to accomplish. Have you tried to contact your local VAR and ask them for assistance? They could at least tell you if you are attempting to use this function as it was intended and if there is a bug, they can help you report it.

 

When trying to get this to work as you would like, I get the same results that you do. There is no G55 fixture offset. I can force it to output a G55 by using tool plane but as expected, it also wants to output an A or C axis rotation.

 

 

 

If you look at the help for each field definition, it is clear that the "Maintain Source Operations" Work offset numbering is only available for the Tool Plane method.

 

Match existing offsets

 

Checks to see if any of the work offset views that are created when the toolpath is posted match any existing or predefined views.

 

If the views match, then the existing view is used.

 

If the views do not match, the new work offset view is created.

 

 

But the Assign New does not say that it is specifically for Tool Plane method of transform.

 

Assign new

 

Creates new work offset numbers for each translation.

 

The work offset numbers begin with the specified Start number and increase by the Increment number with each new translation.

 

 

It may be worth looking in to.

 

I did a rectangular transform using tool plane and it also did "not" output other work coordinates so I would assume that there is an issue.

[Tinhman]

Thanks for your time again.

I think, we may in big trouble with X5 now because we have a ton of programs to run production part using transform operation.

Well,I will email them today.

[neurosis]

I emailed the part file that I created to my local rep. He seems to think that there is an issue and is going to be sending it in to QC. He was not able to get any work offsets other than G54 to output even using tool plane unless the plane itself actually changed, I.E. an axis rotation.

 

It seems as if it is another X5 bug. I also have several parts that we use transform operations on for nesting and they do not output separate fixture offsets. I cant open them and post them in X5.

[Dan@home]

I used the 3X VMC that comes with MC, using the above settings only with 2 instances and ghosting out the source op. It worked fine G54, G55. Mpmaster isn't a 3X post, is maybe the reason?? This a rectangle rotated 0 to 180 deg.

 

N100 G20
N102 G0 G17 G40 G49 G80 G90
N104 T239 M6
N106 G0 G90 G54 X1.3934 Y1.8475 S1069 M3 <<<<<<
N108 G43 H239 Z0.
N110 G1 Y1.3475 F6.42
N112 G3 X1.8934 Y.8475 R.5
N114 G1 X2.5672
N116 G2 X2.8172 Y.5975 R.25
N118 G1 Y-.3173
N120 G2 X2.5672 Y-.5673 R.25
N122 G1 X1.2197
N124 G2 X.9697 Y-.3173 R.25
N126 G1 Y.5975
N128 G2 X1.2197 Y.8475 R.25
N130 G1 X1.8934
N132 G3 X2.3934 Y1.3475 R.5
N134 G1 Y1.8475
N136 Z.2
N138 G55 X1.3934 Y1.8475 Z0.<<<<<
N140 Y1.3475
N142 G3 X1.8934 Y.8475 R.5
N144 G1 X2.5672
N146 G2 X2.8172 Y.5975 R.25
N148 G1 Y-.3173
N150 G2 X2.5672 Y-.5673 R.25
N152 G1 X1.2197
N154 G2 X.9697 Y-.3173 R.25
N156 G1 Y.5975
N158 G2 X1.2197 Y.8475 R.25
N160 G1 X1.8934
N162 G3 X2.3934 Y1.3475 R.5
N164 G1 Y1.8475
N166 Z.2
N168 M5
N170 G91 G0 G28 Z0.
N172 G28 X0. Y0.
N174 M30
%

[Stan_z]

X5 with MPmaster. G54 and G55 ...

 

 

O0001 (T)

(MCX FILE - T)

(PROGRAM - T.NC)

(DATE - JAN-13-2011)

(TIME - 8:14 AM)

(T235 - 1/4 FLAT ENDMILL - H235 - D235 - D0.2500")

N1 G00 G17 G20 G40 G80 G90

N3 G91 G28 Z0.

N5 (COMPENSATION TYPE - CONTROL COMP)

N7 T235 M06 ( 1/4 FLAT ENDMILL)

N9 (MAX - Z.5)

N11 (MIN - Z0.)

N13 M08

N15 G00 G17 G90 G54 A0. X0. Y-1.15 S2139 M03

N17 G43 H235 Z.5

N19 Z.05

N21 G94 G01 Z0. F6.42

N23 G41 D235 Y-1.

N25 X-2.

N27 Y0.

N29 X0.

N31 Y-1.

N33 G40 X.15

N35 G00 Z.5

N37 G91 G28 Z0.

N39 G00 G90 G55 A-180. X0. Y-1.15

N41 G43 H235 Z.5

N43 Z.05

N45 G01 Z0.

N47 G41 D235 Y-1.

N49 X-2.

N51 Y0.

N53 X0.

N55 Y-1.

N57 G40 X.15

N59 G00 Z.5

N61 M09

N63 M05

N65 G91 G28 Z0.

N67 G28 Y0. A0.

N69 G90

N71 M30

[neurosis]

Stan,

 

He/WE are "NOT" looking for an A-axis output. You are rotating the tool path around a plane which is changing the actual tool plane. What he/we are trying to accomplish is separate fixture offset output in the "SAME" tool plane.

 

Example: if you are running several vices on a table and need separate fixture offsets for each vice.

 

Notice that you have an A180. I can get that to work no problem. That is "NOT" the issue.

 

I am assuming that Dan did exactly the same thing that you did only he used a 3 axis post which does not output the axis rotation so it just appears to have worked when in reality it does not.

 

My VAR cant get this to work properly either. There is a definite problem with the transform.

[Stan_z]

IDK.....Maybe it is a bug in rotation only???? cause it works with transform.

 

I'm out that's it for me! Good luck tinhman

[neurosis]

I got confirmation that is was logged as a bug 10 minutes ago.

 

 

Hopefully fixed in MU1.

[neurosis]

IDK.....Maybe it is a bug in rotation only???? cause it works with transform.

 

I'm out that's it for me! Good luck tinhman

 

 

Try setting your transformed path to coordinates and then created a rectangle pattern of the transformed path rather than rotating around a tool plane. You will see that there is an issue.

 

I originally thought that it was operator error and that it was not being used properly. After playing with this for a while I started to realize that it was not just the rotate transform that was not outputting the fixture offsets but that you could not get it to work for nesting or anything else that kept the same tool plane.

[Tinhman]

Good morning Stan_z

It is NOT in ROTATION only, it is in all transform Operation OP.

 

-----------------------------------------------------

Example: if you are running several vices on a table and need separate fixture offsets for each vice.

------------------------------------------------------

 

Please try it with transform/rectangular and let us know if you get G55,G56.... come out in your program and please making sure that your post is supporting 4axis.

[Tinhman]

I am too sloooooooooooooow

 

Thank you Sir!!!!

[Stan_z]

I am too sloooooooooooooow

 

Thank you Sir!!!!

 

 

MP MASTER X5

 

 

 

O0001 (T)

(MCX FILE - C:\AMC\AMC PART FILES\T.MCX-5)

(PROGRAM - T.NC)

(DATE - JAN-13-2011)

(TIME - 2:49 PM)

(T235 - 1/4 FLAT ENDMILL - H235 - D235 - D0.2500")

N1 G00 G17 G20 G40 G80 G90

N3 G91 G28 Z0.

N5 (COMPENSATION TYPE - CONTROL COMP)

N7 T235 M06 ( 1/4 FLAT ENDMILL)

N9 (MAX - Z.5)

N11 (MIN - Z-1.)

N13 M08

N15 G00 G17 G90 G54 X0. Y.7175 S2139 M03

N17 G43 H235 Z.5

N19 Z.05

N21 G94 G01 Z-1. F6.42

N23 G41 D235 Y.5675

N25 X1.6724

N27 Y0.

N29 X0.

N31 Y.5675

N33 G40 X-.15

N35 G00 Z.5

N37 G55 X0. Y.7175 Z.5

N39 Z.05

N41 G01 Z-1.

N43 G41 D235 Y.5675

N45 X1.6724

N47 Y0.

N49 X0.

N51 Y.5675

N53 G40 X-.15

N55 G00 Z.5

N57 G56 X0. Y.7175 Z.5

N59 Z.05

N61 G01 Z-1.

N63 G41 D235 Y.5675

N65 X1.6724

N67 Y0.

N69 X0.

N71 Y.5675

N73 G40 X-.15

N75 G00 Z.5

N77 G57 X0. Y.7175 Z.5

N79 Z.05

N81 G01 Z-1.

N83 G41 D235 Y.5675

N85 X1.6724

N87 Y0.

N89 X0.

N91 Y.5675

N93 G40 X-.15

N95 G00 Z.5

N97 M09

N99 M05

N101 G91 G28 Z0.

N103 G28 Y0.

N105 G90

N107 M30

%